Assemblys and material removal
Assemblys and material removal
(OP)
I have an assembly of two parts. Each part is a separate UG file. I created a new assembly and assembled the parts together (mate, align, etc). Now, to mimic reality, I need to machine a feature in one of the parts. I sketched an outline of my machined feature and then created an extrusion I hoped I could subtract from the part. No go. The option to subtract is not even there.
Question: Is this type of activity not possible in NX5? I assume I'm missing something because other CAD systems have been doing this sort of thing for years.
If not possible, how to I need to approach this sort of design?
Thanks...
Question: Is this type of activity not possible in NX5? I assume I'm missing something because other CAD systems have been doing this sort of thing for years.
If not possible, how to I need to approach this sort of design?
Thanks...
--
Fighter Pilot
Manufacturing Engineer





RE: Assemblys and material removal
Believe it if you need it or leave it if you dare. - Robert Hunter
RE: Assemblys and material removal
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Fighter Pilot
Manufacturing Engineer
RE: Assemblys and material removal
Insert -> Combine Bodies -> Assembly Cut...
It works just like a Boolean Subtract and you don't need to WAVE link or move objects from file to file.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Assemblys and material removal
Any help appreciated. Pro/E experience is hindering ability to use UG. May just give up.
Thanks..
--
Fighter Pilot
Manufacturing Engineer
RE: Assemblys and material removal
Believe it if you need it or leave it if you dare. - Robert Hunter
RE: Assemblys and material removal
Insert -> Associative Copy -> Instance Geometry...
...to make your 'array' and then perform the Assembly Cut operation selecting the multiple tool bodies in your second pick.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Assemblys and material removal
Patience appreciated.
--
Fighter Pilot
Manufacturing Engineer
RE: Assemblys and material removal
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Assemblys and material removal
Not so in UG, where you are working wholly in separate files, that only have a faint appearance of being assembled or related. Try to keep that in mind, and consider that whatever you do it should be possible without being in the assembly.
If you have a complex shaped flange in a base, and need to model a matching flange in a cover, you cant jump into the cover and start making extrudes. You have to wave link a composite curve of the flange profile, or link a face, etc. Then you have enough data in the cover file to start modeling.
When placing a hole thru two parts, if it is for a screw or pin you can model the "false body" in the pin. Perhaps extract the body and offset the diameter for clearance using direct modeling, then link that body into each component and subtract it. I havent had a chance to use the new 'hole series' feature yet, but have created holes in the first part with the boolean set to none, then that body into the second part before subtracting it from both.
NX 5.0.3.2 MoldWizard
RE: Assemblys and material removal
I've been having a difficult time moving over to UG. I moved to CATIA V5 with ease but I just cannot figure out what UG is looking for sometimes. I've asked people here about how to do certain things in UG as I did in Pro/E and I get the "glassy eyed" look most of the time. I told them about Pro/E's ability to "show" dimensions when doing a drawing and you'd swear I was speaking in a different language.
Someone tried to explain to me what I needed to do in the assy to make machined cuts and I ended up glassy eyed. The NX "Product Evangelist" in this forum has helped me understand but it still seems way more difficult than the way Pro/E approached the issue. I didn't have to think of boolean operations in Pro/E as it was all handled in the background.
Hopefully this won't start a Pro/E v. UG discussion but I'm just trying to understand some of the underlying ways UG does things.
--
Fighter Pilot
Manufacturing Engineer
RE: Assemblys and material removal
Believe it if you need it or leave it if you dare. - Robert Hunter
RE: Assemblys and material removal
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Assemblys and material removal
NX has its roots in legacy non-parametric modeling, leveraging that can be a real boost in productivity.
For example, in a mold design when a customer sends a changed part model it must be added to the assembly. Its coordinate system is way out in space someplace, and the part may not have good geometry or datums to make assembly constraints (mate, etc). You can assemble the new model inside the old part model using the absolute csys, then go back to the top assembly and drag the new model out to wherever you want it in the assembly tree, and delete the old model. It keeps its position/orientation. No need to reposition, move, or constrain it.
Sketch profiles/section curves, extruded bodies, and boolean operations are all (mostly) separate where proe combined them in a single step. I like this way, as I create VERY few sketches anymore. I do a lot of simple lines, say from midpoint 1" along the Y axis, then extrude that.
If you have any specific questions or examples I can try to elaborate more.
NX 5.0.3.2 MoldWizard
RE: Assemblys and material removal
-Dave Tolsma
Tolsnet LLC
http://groups.google.com/group/NX_CAX/
http://groups.google.com/group/plm-exchange/
RE: Assemblys and material removal
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Assemblys and material removal
Can you explain why I just cannot "show" dimensions of my features in a drawing ala Pro/Engineer? Am I missing something?
Thanks...
--
Fighter Pilot
Manufacturing Engineer
RE: Assemblys and material removal
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.